The SPRINGBACK under Process template is used to simulate the springback of the blank after drawing simulation, as shown in Figure 8.2.103. The user can also add springback stage in multi stage simulation, as illustrated in Figure 8.2.104. Springback process consists of four pages. For information about General and Blank, refer to Section 8.2.4 Forming.
Figure 8.2.103 Springback analysis
Figure 8.2.104 New springback stage
The Blank page is illustrated in Figure 8.2.105, The gravity load option in Process page enables the user to consider the influence of gravity in springback analysis. This option is not toggled on by default.
Figure 8.2.105 Process definition page
CONSTRAINT
The user can select Inertia Relief or Single Point Constraints when setting springback constraint. Inertial Relief uses rigid body mode to analyze linear static problem.
Inertia Relief
Selecting Inertia Relief to analyze springback, the user can set a threshold value and the default is 0.001Hz.
Single Point Constraints (SPCs)
Allow the user to select three nodes to constrain rigid displacement of blank during springback analysis. The first selected node is constrained in X, Y, Z direction. The second selected node is constrained in Y, Z direction. The third selected node is constrained in Z direction. The relationship of location for these three constraints is illustrated in Figure 8.2.106.
Figure 8.2.106 Springback constraints definition
Nodal Forces
The user may apply force on node. The setup dialog box for nodal forces is illustrated in the Figure below. In the nodal forces list, FC indicates constant force, and FV indicates force which varies with time.
Figure 8.2.107 Nodal forces
Force
The user is allowed to apply FC or FV on the selected nodes.
Direction
The user is allowed to define the force direction, and the default direction is +W.
New: Select node to apply nodal forces.
Modify: Modify the force and direction of the selected node.
Delete: Delete the nodal force of the selected node.
Delete All: Delete the nodal forces of all the defined nodes.
OK: Accept the defined nodal force and exit.
Cancel: Do not accept the defined nodal force and exit.
Set control parameters for springback analysis, as illustrated in Figure 8.2.108.
GENERAL
SHELL WARPING STIFFNESS (BWC): Default is set as 2, i.e. Belytschko-Tsay
ADVANCED: Advanced parameter setting.
Figure 8.2.108 Springback control parameters interface
IMPLICIT ANALYSIS
Allow to user to select approach of springback analysis: single step springback or multiple step springback analysis. Multiple step springback is set as default option. Single step springback analysis usually leads to good result. However, converged result may not be obtained using single step springback analysis for relatively flexible part. The user is recommended to conduct springback analysis using multiple step approach. Detailed descriptions for setting up single or multiple step springback analysis is described in LS-DYNA User’s Manual.
INITIAL TIME STEP SIZE (DT0): Initial time step size of springback analysis. Default value is 0.001.
NUMBER OF IMPLICIT STEP (NSBS): Number of implicit step. Set to 1 if single step implicit analysis is performed. If the value is greater than 1, multiple implicit analysis is used.
ADVANCED: Set advanced parameter of implicit analysis. See Figure 8.2.109 for the list of parameters.
Figure 8.2.109 Advanced parameter for Implicit Analysis
COARSENING MESH
Allow the user to use coarsening mesh technique during springback analysis. During drawing simulation, adaptive mesh is adopted to refine blank mesh to capture details on tooling. Adaptive meshing increases model size and posses challenge to the convergence in springback analysis. This option merges the refine mesh on the flat areas to reduce model size. It reduces convergence problem and shorten the computing time.
ANGLE: Set the angle criteria for merge neighboring elements. If difference of element normal angle between adjacent elements is less than the given criteria, these elements are merged. Default angle is 8°.
CHECKING MESH
This function allows the user to check mesh quality during Springback analysis. The user can check adaptive constraints, minimum aspect ratio, minimum and maximum allowable interior angle and minimum element size.
FIXING BAD ELEMENT
This function enables solver to automatically repair distorted elements and output the relevant information into text file. It helps to increase precision of springback analysis, as well as improving convergence.